Hello Brendon,
Thank you for your response to my question.
It is logical that all modules have a unique RefDes. When I spoke to Christi
Cassares at the Protel Customer support she showed me how to easily update
the RefDes from U1 to U1_1.
(all RefDes are set as ?)
copy the module as many times as needed, then goto
>>TOOLS>>ANNOTATE>>ADVANCED OPTIONS and you can set the suffix for each
sheet as needed. I found this was the easiest way of annotating each sheet.
Coming from a beginner to Protel I hope this helps anyone who did not know
of this.
As for my problems with ports and net labels, that was my problem..... I
forgot to change the names of all the ports in my modules when I converted
from complex to simple hierarchy. They all shared the same net therefore
giving me a wrong "rats-nest".
Very kind regards,
Bryan Bernesi
-----Original Message-----
From: Brendon Slade <[EMAIL PROTECTED]>
To: Multiple recipients of list proteledausers
<[EMAIL PROTECTED]>
Date: Monday, February 12, 2001 3:25 PM
Subject: Re: [PROTEL EDA USERS]: complex Multi-level schematics...
Hi Bryan.
> I am making a multi-layer board (2 signal, 2 power)
> with 24 exact modules.
Even when you have repeated modules within a design, at the very least
component designators have to be unique. If you're not using "Ports only
Global" or "Sheet Symbols/Port Connections" then your netnames (where
required) need to be unique also.
> Each module has an isolated power and ground as well
> as two signal nets. (which are connected with net labels and ports)
> Now, When I run >>TOOLS>>UPDATE PCB (with NET LABELS AND PORTS GLOBAL
> enabled), all of my nets are connected except for the isolated power and
> ground, and my 2 signal nets.
(ref. P130 and P135 of Protel99se Designer's Handbook)
If you're using "Net Labels and Ports Global" then all nets with the same
name will be joined. As a preference I use "Sheet Symbols/Port Connections"
and any signals that I wish to go off the sheet I attach to a port. I
always have a top sheet that shows the connectivity of the individual
sub-sheets. An easy way of getting the porting info from the sub-sheets is
to have the top sheet current, select "Design | Create Symbol From Sheet" in
the schematic editor, select which sheet you wish to show on this top sheet,
then place it. Repeat this for as many sheet as you require. Protel gets
the porting info from the sheet you selected. Now just connect the relevant
ports with wires and/or busses where appropriate. Now run "Tools | Update
PCB | <Sheet Symbols/Port Connections>" and see how that goes.
> Also, each module has to be placed and wired the same way. No problem, or
so
> I thought. I placed the components and wired the first module; ran the DRC
> no problems. I Copied it, and pasted it (using >>EDIT>>PASTE
SPECIAL>>PASTE
> ARRAY), great.... no problems so far, once I had all 24 modules placed I
ran
> a DRC again and I get clearance and short-circuit constraints. why????
I think Abd ul-Rahman Lomax wrote a good explaination of this, however, I
think he omitted the "Paste Special | Duplicate Designator" option,
otherwise Protel will automatically assign unique numbers to all pasted
components.
> On another note, sometimes when I run the ERC some of my symbols are
changed
> in my schematic, i.e.
> I have a PNP transistor (2N2904 symbol labeled as a TIP125) that changes
to
> a different transistor symbol (taken from ????), or a LED (a created
symbol)
> that changes back to the standard LED symbol (found in miscellaneous
> devices.lib) but the LED symbol does not change in all 24 modules?!?!?!?!
I have no idea, except maybe check on the libraries you have open, and
remove the standard Protel one.
Hope this helps.
Brendon.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* This message sent by: PROTEL EDA USERS MAILING LIST
*
* Use the "reply" command in your email program to
* respond to this message.
*
* To unsubscribe from this mailing list use the form at
* the Association web site. You will need to give the same
* email address you originally used to subscribe (do not
* give an alias unless it was used to subscribe).
*
* Visit http://www.techservinc.com/protelusers/subscrib.html
* to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
* This message sent by: PROTEL EDA USERS MAILING LIST
*
* Use the "reply" command in your email program to
* respond to this message.
*
* To unsubscribe from this mailing list use the form at
* the Association web site. You will need to give the same
* email address you originally used to subscribe (do not
* give an alias unless it was used to subscribe).
*
* Visit http://www.techservinc.com/protelusers/subscrib.html
* to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
________________________________________________________
To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'
More Information : http://www.dolist.net